Home>Forum>Topic
Latest Topics Latest Replies EasyEDA Std EasyEDA Pro JLCPCB LCSC OSHWLAB General Discuss
PCB SMT 3D/CNC Feature Requests Bug Reports
You need to use EasyEDA editor to create some projects before publishing
Two PTH in oval pad, one hole oval, is this acceptable?
1769 6
david.stosik 4 years ago
Hello, I'm trying to design a PCB on which I would like to have two plated through-holes, one of them being oval, sitting on the same pad (or at least connected by a trace). Is such design acceptable, following JLCPCB's capabilities? I noticed this thread: [Oval pad with two holes](https://easyeda.com/forum/topic/Oval-pad-with-two-holes-99871d6c373148f5909d2c322087ad31), which gave me some answers, and I also checked [JLCPCB's capabilities](https://jlcpcb.com/capabilities/Capabilities), but I am still unclear whether the dimensions I am using are acceptable... I would really appreciate getting your input on this. Here it is in "resources": [OVALPAD2HOLES](https://easyeda.com/component/3aa3c1a4a9e14ff494c3d62b933e9612), and this is what it looks like: ![image.png](//image.easyeda.com/pullimage/msRUzm5CYboeqAZW5okF4wOYgIPG6zUPLnK885UY.png) Thanks in advance for your very precious help. Update: I learned that I can edit a post, but I cannot edit/delete a reply. So I'll put the additional info here too: I noticed this rule in JLCPCB's capabilities: > The minimum plated slot width is 0.65mm, which is drawn with a pad. The slot in the screenshot above was only 0.6mm wide, so I increased it, as well as the round hole diameter, to 0.65mm. I kept both annular rings to 0.4mm, so the two holes are still 0.8mm apart. You can check the updated [OVALPAD2HOLES](https://easyeda.com/component/3aa3c1a4a9e14ff494c3d62b933e9612) resource. ![image.png](//image.easyeda.com/pullimage/iD4S8kMaUrZ8IJ10zb9ThGqBs8dUxsu8CDqOBbJa.png)
Comments
david.stosik 4 years ago
Update: I noticed this rule in JLCPCB's capabilities: > The minimum plated slot width is 0.65mm, which is drawn with a pad. The slot in the screenshot above was only 0.6mm wide, so I increased it, as well as the round hole diameter, to 0.65mm. I kept both annular rings to 0.4mm, so the two holes are still 0.8mm apart. You can check the updated [OVALPAD2HOLES](https://easyeda.com/component/3aa3c1a4a9e14ff494c3d62b933e9612) resource.
Reply
andyfierman 4 years ago
@david.stosik, It looks like you have correctly made this as a PCB footprint  with all parts connected by pads rather than just a couple of pads joined by a trace, so I'm guessing that you have already found this, but just in case you have not: [https://easyeda.com/forum/topic/How-to-avoid-DRC-errors-when-connecting-to-PCB-Footprints-a-k-a-PCB-Libs-90bf944fe3644b21a7d27a9e9d8df8d6](https://easyeda.com/forum/topic/How-to-avoid-DRC-errors-when-connecting-to-PCB-Footprints-a-k-a-PCB-Libs-90bf944fe3644b21a7d27a9e9d8df8d6) Note that unless you add solder mask back in between the Multi-layer pads, the Top Layer pad between them will also be exposed copper. You can close the solder mask aperture in the Top Layer pad by setting a negative solder mask expansion of a value equal to or greater than half the smallest dimension of the pad (in this case the width) so if the pad is 1.4 mm wide, set the solder mask expansion to -0.7mm.
Reply
david.stosik 4 years ago
@andyfierman  Thanks a lot for that link, I'm sure I'll learn a lot from it! > Note that unless you add solder mask back in between the Multi-layer pads, the Top Layer pad between them will also be exposed copper. Very nice catch, thanks for the advice! I did a few tries: ![image.png](//image.easyeda.com/pullimage/br6gBeHkyQJfZq5Fr3MHr91VBXhHkdDAmEhDziX9.png) * U1: * solder mask expansion is 0 on the multi-layer pads (the holes) * solder mask expansion is 0.1mm on the top-layer pad (the big oval) * U2: * solder mask expansion is 0 on the multi-layer pads (the holes) * solder mask expansion is -1.0mm on the top-layer pad (the big oval) * U3: * solder mask expansion is 0.1mm on the multi-layer pads (the holes) * solder mask expansion is -1.0mm on the top-layer pad (the big oval) * U4: * solder mask expansion is 0.05mm on the multi-layer pads (the holes) * solder mask expansion is -1.0mm on the top-layer pad (the big oval) It took me a while to see it as it is (a thin blue lacquer-like layer is applied on top, some copper, some non-copper areas), but I'm not sure whether one option is clearly better than the others. Is there any you would recommend?
Reply
andyfierman 4 years ago
Check the results in the Gerber files but if you close off the solder mask for the single layer pad then the apertures for the round and oval pads will still expose the multi-layer pads whilst leaving the rest of the single layer pad area covered in solder mask. Obviously can choose what aperture suits your application.
Reply
david.stosik 4 years ago
This is what I went with: [SPRINGPAD](https://easyeda.com/component/68f53ab82d414710855f891d373a3de4). If anyone's interested: don't forget to set a negative paste mask extension on the top (and bottom) single-layer pads (the connecting ovals) in order to remove the whole area from the stencil, shall you need one. I'm now trying to understand how to use this PCBLib in a project's PCB or PCB module in a way that does not require me to change four items' "number" every time I add a SPRINGPAD to my PCB. (I'm planning to have 16 or 22 SPRINGPADs on my board, and would like not to have to renumber 84 items on the board. 😬 )
Reply
andyfierman 4 years ago
If you mean that you want to have n instances of SPRINGPAD in the Schematic and therefore on the PCB then the Editor will take care of any renumbering because they will be prefixed something like SP1, SP2, SP3...SPn in the Schematic and hence the same in the PCB so you don't need to worry about renumbering the pads. If you mean that you want to have n instances of SPRINGPAD in a PCB Footprint (a.k.a. PCBLib) then it may be easier to construct n sets of elements in the PCBLib Editor starting with all the round holed pads then all the slotted pads then all the top layer pads because once a pad has been defined, its properties are inherited for all subsequently placed pads and the numbering incremented (not when copying and pasting however). Then you can use the **Format > Distribute Array** tool for each set of elements to place them exactly. It might be easier to just copy and paste all the Top layer pads onto the bottom layer as the last step since by then they will have right pad numbering and in the right relative positions.
Reply
Login or Register to add a comment
goToTop
你现在访问的是EasyEDA海外版，建议访问速度更快的国内版 https://lceda.cn(需要重新注册)
如果需要转移工程请在个人中心 - 工程 - 工程高级设置 - 下载工程，下载后在https://lceda.cn/editor 打开保存即可。
有问题联系QQ 3001956291 不再提醒
svg-battery svg-battery-wifi svg-books svg-more svg-paste svg-pencil svg-plant svg-ruler svg-share svg-user svg-logo-cn svg-double-arrow -mockplus- -mockplus- -mockplus- -mockplus- -mockplus- -mockplus- -mockplus- -mockplus-@1x -mockplus-

Cookie Notice

Our website uses essential cookies to help us ensure that it is working as expected, and uses optional analytics cookies to offer you a better browsing experience. To find out more, read our Cookie Notice